In Kicad, the PCB layout / schematic editor I use there is an option to export Gerbers in 4.5 or 4.6 format. I can not find any documentation on what this means. Any help would be appreciated.
This basically controls the number of digits before and after the decimal point in the Gerber output (if you're not omitting leading or trailing zeroes):
4:4 -> 0034.5678
So basically, 4:4 will give you 0.1um resolution, 4:3 will give your 1um resolution, ...
The 4:4 or 4:5 or any other 4:x format is used when you output your Gerbers in [mm]. If you're using imperial numbers, you will typically have something like 2:x.
Using Gerber a format 4.5 means four decimal digits before the decimal point and five digits after the decimal point. This may be done using mm or inch as unit.
But using 4 digits before the decimal point and mm as unit, a board of 9.999 m length may be done. For boards shorter than one meter, 3 digits will do. Using inch, 2 digits will do.
For a precision of 1 µm using metric units, 3 digits after the decimal point will do and for a precision of 0.1 mils using imperial units 4 digits are enough.
But the Gerber format may have problems with numeric instabilities when arcs are used, Ucamco recommends 5 or 6 digits after the decimal point to avoid those numeric instabilities.
Another feature is the supression of leading or trailing zero supression. If a number format 3.6 is used, the value 012.340000 with leading zero supression will output 12340000 and trailing zero supression 01234. The trailing zero omission is deprecated and only leading zero omission should be used.
There was also absolute or incremental notation, but nowadays the incremental format is deprecated and only the incremental format should be used.